open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I have an enclosed tidal region (fjord area) and I want to use Thompson boundary condition for the one open boundary I have together with a time-varying free surface value (free velocity). The rest of the domain has solid boundary with velocity set to null.
Using the classic boundary condition works fine, but Thompson doesn't work at all. The simulation takes very long time, and for the few time-steps I can view, the results are not good with unrealistic high values of both velocity and free surface.

My questions are:
1. What could be wrong?
2. Thompson is the recommended method to use for a tidal area, but is it then wrong to use the classic boundary condition?

Thank you
Emilia

Hi Emilia,

Which version of TELEMAC-2D are you using?
Before Thompson's theory was revisited by Jean-Michel (Hervouet) in version 6.1 (so that it can be used in parallel, please see the proceedings of the 18th TELEMAC-MASCARET User Club), there was a big difference for time computations if using Thompson or not (something like 8 times if I remember). In parallel with version 6.2, I have not noticed such differences (even though a little bit faster without Thompson's conditions).

In my proper experience, Thompson conditions work better if you have both elevation and velocities values.
When running simulations with only elevation without Thompson's conditions, I got results that are not so far from simulations with both elevation and velocities and with Thompson's conditions, except close to the open boundaries and some warning messages such as
'ILL-POSED PROBLEM, ENTERING FREE VELOCITY
FOR EXAMPLE AT BOUNDARY POINT NUMBER'
The problem occurs in particular when the current is directed inwards on the open boundary though prescribing elevation.

I would say that if you are far from the open boundary, your result is OK with classic boundary condition.

Perhaps Jean-Michel or someone else will be able to complete this answer.

Hope this helps,

Chi-Tuan

PS: if your area is covered by one local tidal solution provided by Oregon State University (e.g. European Shelf or Iceland)
volkov.oce.orst.edu/tides/region.html
perhaps, you can try to use the new developments of TELEMAC 6.2 to deal with these databases of harmonic constants? OSU provides both elevation and velocity values for open boundary conditions, so that Thompson's conditions can be used.

Thank you for your quick reply.
I am using version 6.2, but as you say, I'm not interested in the result close to the boundary so I leave it with the classic boundary condition.

I'm getting a lot of notification about the that my maximum iteration is exceeded. I think it is due to my imposed surface level. Should I be worried if the relative precision is <0.005? The simulation time is quite large

Thank you for your help

Hi again,

Before investigating further, can you send your steering file + Fortran file, please?
You can also read the topic "Tidal model with v6p2" where you can find some advice for a steering file with modelling of tides
www.opentelemac.org/index.php?option=com...t=32&Itemid=177#6164

If your maximum number of iterations is exceeded, this means that you do not solve your equations with a good accuracy. 0.005 for relative precision does not sound so good.

Please send your steering file, perhaps it can be improved with better options.

Regards,

Chi-Tuan

Hi Emilia,

In addition to my previous post, in the validation directory, you can have the test case 123_tide which can give you some better options for your steering file to accelerate your computation (in particular TREATMENT OF THE LINEAR SYSTEM = 2, with the choice of the associated solver SOLVER = 1, MATRIX STORAGE = 3, TYPE OF ADVECTION = 1,5, DISCRETIZATIONS IN SPACE = 11;11 with FREE SURFACE GRADIENT COMPATIBILITY < 1.).

Hope this helps,

Chi-Tuan

Hi!

I noticed I had put on the option for tidal flats, even though this is not interesting for me. When removing this option, the computation is faster.

With a time step of 50, as I have in my model right now and approximately 15000 or more (I will change that later) number of time steps, anything that help to speed up the computation will be appreciated.

I have not used a fortran file, instead I have a time-varying surface elevation file. I attach both.
Thank you again

and this file with a modified extension

Hi again,

I have several remarks that may help you:
You are using DISCRETIZATIONS IN SPACE = 12;11 which corresponds to quasi-bubble elements for velocities (a type of finite element intermediate between linear and quadratic, with one extra degree of freedom compared to classical triangular P1, please see manuals or Jean-Michel Hervouet's book). This costs a lot compared to 11;11 (P1). If you use 11;11, to avoid spurious oscillations, you should use FREE SURFACE GRADIENT COMPATIBILITY = 0.9 or less.
As advised in my previous post, you should use TREATMENT OF LINEAR SYSTEM = 2 (wave equation) with SOLVER = 1 (conjugate gradient) as the system is symmetric. That enables to accelerate the computations. Then, the default accuracy (1.E-4) or less may be reached.
At last, if you have one or more multi-core processors, you can use parallel computation which allows you to decrease your computation time a lot if your domain is large enough (PARALLEL PROCESSORS = 8 e.g. for two quad-core processors).

Moreover, I have a few remarks that will not decrease your computational time a lot (or at all):
you can increase your GRAPHIC PRINTOUT PERIOD if you only need results at a longer period (e.g. 12 to have it every 10 min for a time step = 50. s). So does LISTING PRINTOUT PERIOD.
The keyword STEERING file is not necessary (and may be tricky if it is not the same as the real name of your steering file).
One physical remark: if your domain is large, do not forget to activate CORIOLIS keyword and calculate CORIOLIS coefficient (please see the help in the dictionnary to calculate it).

Just for my information, why have you chosen SUPG OPTION = 1;2 those of IMPLICITATION FOR DEPTH or VELOCITY = 0.6, and SOLVER = 3?

Hope this helps,

Chi-Tuan

Hi!

Thank you for your quick replies!

As I am new to Telemac, I began using the cas-file for the Mersey estuary where they have chosen the options you commented on. I'm still working on getting things to work so I haven't changed any of these options yet.

I will try again with your recommended settings.
Thanks!

The simulation works excellent and it is very fast. Thank you again.

I wonder if I should worry about error such as "I'll posed problem ...entering free velocity". Here it is said at boundary point 1314-1316 which is part of the liquid boundary. I have set the velocity to "constant at the boundaries/variable in time" (in Fudaa) so the notice confuses me.